Person using fully define sketch in SOLIDWORKS

How and when to use Fully Define Sketch in SOLIDWORKS

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 For some projects, it’s important to fully define your sketches in 3D CAD programs because it helps reduce errors and ensures the geometry stays the same. There are some great arguments for when to use and when not to. In General, Fully Define Sketch in SOLIDWORKS is a handy way to fully dimension your sketch. When modeling in SOLIDWORKS, it’s nearly always best practice to fully define sketches before moving to the next step or feature of the model. For example, sketches for rib features can typically be left under-defined, as well as temporary sketches used for quick tests. 

While sketches can be fully defined manually and in a variety of ways, the Fully Define Sketch tool can be used to quickly add many dimensions and/or relations to a sketch at once to fully define it. 

Know When to Use Fully Define Sketch vs. When to Dimension Manually

While the decision ultimately rests with each user and his or her preference and sometimes the type of design you are working on, two things should be kept in mind when deciding whether to use the Fully Define Sketch tool or to dimension manually:  

  1. Consider how many dimensions or relations need to be added to a sketch. 
  2. Consider how close the Fully Define Sketch tool will get to the desired result.  

Typically, as the number of dimensions or relations increases, especially if they are repetitive, it becomes more advantageous to use the Fully Define Sketch tool.  

Additionally, the geometry of the sketch will determine how close the Fully Define Sketch tool gets to the desired result. If the sketch contains more complex geometry like arcs, splines, and ellipses, or requires relations like equal or midpoint, it is typically better to define these items first before running the tool. If the sketch contains lines and points, and relies on relations like horizontal/vertical, parallel/perpendicular, and coincident, it will be more suited to the Fully Define Sketch tool. 

4 Useful Examples of Sketches when Using Fully Define Sketch 

Here are some example sketches showing what to look for when determining if the Fully Define Sketch command will work well. 

Example #1: Use Fully Define Sketch with a Grid of Lines 

Using fully define sketch with grid of points

Figure 1: A grid of points is an example of where the Fully Define Sketch tool works well. It creates and arranges dimensions and adds relations between horizontal or vertical points to eliminate redundant dimensions.

Example #2: Use Fully Define Sketch with a Single Closed Contour of Lines 

Using fully define sketch with a single closed contour of lines

Figure 2: A single closed contour made of lines is another example where the Fully Define Sketch tool works well. However, it will only add horizontal or vertical dimensions, not aligned dimensions or angles.

Example #3: Avoid Ellipses with Fully Define Sketch 

Avoid ellipses if using fully define sketch

Figure 3: Ellipses do NOT work well with the Fully Define Sketch tool. The ellipse on the right was sketched with a horizontal alignment, which the tool correctly added relations for. However, the remaining dimensions are cumbersome to work with as they d

Example #4: Use Fully Define Sketch in Combination with Manually Defining Relation 

Use fully define sketch in combination with manually defining relation

Figure 4: A closed contour made of lines and arcs works alright, but the tool will dimension the arcs separately. To control the arc radii with a single dimension, an equal relation can be added manually before running the tool.

How to use Fully Define Sketch in SOLIDWORKS

Below, the Fully Define Sketch PropertyManager will be covered, where all the different settings of the tool can be adjusted. The sketch below will be the example used in this section. 

Example sketch in SOLIDWORKS

Figure 5: This is the example sketch that will be used in the next sections. The numbering has been added for clarity. Lines 3 and 7 are aligned, but no relation exists between them. Lines 1 and 8 are coincident to the origin. All lines have either a hori

How to access the fully define sketch command in SOLIDWORKS

Figure 6: The Fully Define Sketch command is accessed using the drop-down arrow beneath “Display/Delete Relations.” It will only appear while editing a sketch that is not already fully defined.

Select Which Entities to Fully Define 

The first section of the PropertyManager controls which entities the tool has access to: either all entities or only selected entities. Use selected entities if you want to manually define parts of your sketch after running the tool. Use all entities if you want to fully define the sketch and any manual dimensions or relations (if necessary) have already been added.  

Relations 

Select which relations to apply in the PropertyManager

The second section of the PropertyManager controls which relations the tool may add to the sketch. Selecting these relations only makes them available for the tool to use in its calculation but does not guarantee it will use all of them or even any of them. Checkboxes exist to quickly select or deselect all available relations, or individual relations can be clicked to toggle them on or off. 

In the example sketch, because the top lines 3 and 7 are aligned with each other, a collinear relation will be added by the Fully Define Sketch tool if the relation is enabled. See the example images below. 

Turn on relations when using fully define sketch in SOLIDWORKS

Figure 7: With relations turned on, a single vertical dimension controls both lines 3 and 7 at the top, and a collinear relation is added between the lines.

Turn off relations when using fully define sketch in SOLIDWORKS

Figure 8: With relations turned off, two vertical dimensions are added, one for line 3 and one for line 7, so they can/must be controlled independently.

Note that relations will only be added by the Fully Define Sketch tool if the entities are already in the proper position. In this example the lines were already collinear (because of their initial snapping with inference lines), so a collinear relation could be added. These alignments can be achieved by using the blue inference lines to snap sketch geometry to the proper position while sketching. 

Dimensions 

Dimensions panel in SOLIDWORKS

Last is the dimension section. The scheme can be selected in the horizontal and vertical directions as either chain, baseline, or ordinate. See the pictures below for examples of each scheme. 

Chain Dimensioning Scheme  

Chain dimensioning scheme in SOLIDWORKS

Figure 9: The chain dimensioning scheme. Note that the last (rightmost for horizontal dimensions, or topmost for vertical dimensions) dimension will appear as an overall length instead of a chain. (The 156.17 horizontal dimension or the 78.60 vertical dim

Baseline Dimensioning Scheme  

Baseline dimensioning scheme in SOLIDWORKS

Figure 10: The baseline dimensioning scheme. A separate dimension is inserted and automatically arranged from the datum (the origin in this case) to each entity.

Ordinate Dimensioning Scheme  

Ordinate dimensioning scheme in SOLIDWORKS

Figure 11: The ordinate dimensioning scheme. This effectively works the same as baseline, but the arrangement is a little different. Works especially well when there are many dimensions next to each other.

Datums when Using Fully Define Sketch  

Datums in baseline dimensioning scheme in SOLIDWORKS

Figure 12: This is the same baseline dimensioning scheme shown before, but the datums have been changed from the origin to the pink (horizontal datum) and purple lines (vertical datum)

The datums control where the horizontal and vertical dimensions are measured from. They can be either internal to the sketch (a point or line in the sketch), or external to the sketch (the origin, or a model edge or vertex). When using a datum attached internal to the sketch, the size and shape of the sketch can still be fully defined, but its position relative to the part origin may not be defined. See the example sketch below. 

Sketch with datum set to the origin and sketch fully defined in SOLIDWORKS

Figure 13: Datum is set to the origin; sketch is fully defined.

Sketch with datum set to the lower left corner and sketch under-defined in SOLIDWORKS

Figure 14: Datum is set to the lower left corner of the rectangle; sketch is under-defined because the rectangle is still free to move relative to the origin.

Dimension Placement when Using Fully Define Sketch  

Changing dimensions to above sketch or right of sketch in SOLIDWORKS

Figure 15: The positions of the dimensions here have been changed to “Above sketch” for horizontal and “Right of sketch” for vertical.

Example Walkthrough of Using Fully Define Sketch  

  1. Create a sketch, making use of inference lines to capture any basic relations (horizontal, vertical, perpendicular, parallel) 

Example of a sketch to fully define in SOLIDWORKS

       2. Choose “All entities in sketch” 

Choose All entities in sketch in SOLIDWORKS

      3. Enable all relations 

Enable all relations SOLIDWORKS

       4. Choose the desired dimension scheme (Ordinate, in this case) 

Choose desired dimension scheme in SOLIDWORKS

       5. Change the datum, if desired. For this example, the datum will be changed to the lower left corner of the sketch. 

Change datum if desired in SOLIDWORKS

       6. Click the “Calculate” button to preview the results.  

Click calculate in fully define sketch in SOLIDWORKS

       7. Evaluate the results. In this example there are two problems: First, the sketch is still under-defined because it has no dimensions controlling its position relative to the origin, and second, the two arcs are dimensioned separately while the design intent calls for them to be equal. From here there are three options at the top of the PropertyManager. (Just above the Entities to Fully Define section) 

    1. Green check: Accept the results as-is and insert them into the sketch 
    2. Red X: Discard the added dimensions and relations and go back to editing the sketch manually 
    3. Blue arrow: Discard the added dimensions and relations and go back to the PropertyManager to adjust any settings which may give a better result (e.g. changing datums, enabling/disabling relations)

       8. For this example, we will discard using the red X and go back to manually editing the sketch. 

       9. Manually add an equal relation between the two arcs. 

Manually adding equal relations in a sketch in SOLIDWORKS

       10. Rerun the Fully Define Sketch tool. The radii are now controlled by a single dimension, but the sketch is still under-defined because there is no relation or dimension to the origin. 

SOLIDWORKS under-defined info panel while using fully defining sketch

       11. Green check to accept the results as-is. 

       12. Manually add dimensions to position the sketch relative to the origin and fully define it. 

Manually add dimensions in SOLIDWORKS

       13. Adjust any remaining dimensions to their final values by double clicking each one and inputting the desired value 

Adjust remaining dimensions in SOLIDWORKS

Common Pitfalls

After completing the Fully Define Sketch command with the green check, the only way to revert is to use undo (Ctrl-Z). Make sure you do not continue working unless you are satisfied with the results of the tool (e.g. adding more dimensions, relations, sketching) as any work you do after the tool will need to be undone if you decide you want to undo the actions of the Fully Define Sketch tool. 

A workaround (which is nearly as quick) to this is to manually delete the dimensions and/or relations added by the tool instead of using undo. 

Final Thoughts on Fully Define Sketch

The Fully Define Sketch tool is very powerful and can be used to save both time and effort when working in SOLIDWORKS. However, like most tools, knowledge of when it’s best applied is as important as simply how to use the tool. Based on the examples shown here, you should be able to develop your understanding of the tool and determine at a glance which of your sketches are best suited to the tool and which sketches should be manually defined.

If you have any questions about this tool or other time-saving tips in SOLIDWORKS, contact us today. 


Picture of Kenny Truong

Kenny Truong

Kenny Truong is an Applications Engineer based out of our Brooklyn Park, MN office. He comes from a background of engineering at a local startup and student teaching at the University of Minnesota. He specializes in SOLIDWORKS 3D modeling.
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